Waterline toolpath

[KMartin]

Hi Everyone - Could I please get some help with this waterline toolpath . This is not the actual part

I'm machining  put the surface is identical  . The surface starts 2.5 inches below top of part so

i'm not able to use a contour because surface goes to deep and also the splines don't make for a good finish .

I need to get about a 63 finish if possible . The machine is a hass . On the trial cut the finish was choppy .

Tried to tighten up tolerance  but not much improvement . Also the part is a rush job like most of the stuff

we do .I have never tried machining with a solid would that help at all  .Thanks for any help in advance . 

 

 

The file is saved under ftp://ftp.mastercam-cadcam.com/Mastercam_forum/X9_Files/waterline

[goooose]

I would use a contour. Just create a silhouette boundary to get arcs to drive the toolpath. Increase the tolerance to get larger arcs...maybe 0.002?

Might be a better way...?

[Reko]

Well, if surface finish is what you're after, you need to adjust your filter settings.

 

I adjusted the filter on your program and posted the code... your program was just under 5,000 lines... my program was nearly 310,000 lines long.

 

You will definitely need to have high-speed-machining on your Haas, but you can try these settings:

 

 

 

[KMartin]

We have high speed machining but program cannot be bigger than 1 meg 

[crazy^millman]

We have high speed machining but program cannot be bigger than 1 meg 

 

This may not be taken well, but time to get a new machine. I have some roughing programs that are 120mb.

[Reko]

We have high speed machining but program cannot be bigger than 1 meg 

You can easily DNC that program from your computer. Mastercam comes with Cimco, a file editor and communication program, and your Haas can be set up to run right from your computer no matter how big the file is.

[KMartin]

I would use a contour. Just create a silhouette boundary to get arcs to drive the toolpath. Increase the tolerance to get larger arcs...maybe 0.002?

Might be a better way...?

 

 

Thanks   goooose   that  did the trick .

• Like This

•  Back to top
•  Quote
•  MultiQuote
•  Report

[Reko]

 

Thanks   goooose   that  did the trick .

Yep... you can always go old school... sounds like you will have to avoid a lot of the newer HS toolpaths as most of them require a lot of extra code.

[cool]

Hi,

how old is your HAAS? Does your HAAS has a USB port on the control? You can feed your program from the USB stick. Is your machine setting in the control at fine corner rounding 0.005?

[KMartin]

Hass machines are pre 2000 .Still using a floppy disk .Machine setting is set at .025 . As I understand it corner rounding will start .025 from corner .

Mastercam will  set accuracy . 

[Reko]

Hass machines are pre 2000 .Still using a floppy disk .Machine setting is set at .025 . As I understand it corner rounding will start .025 from corner .

Mastercam will  set accuracy . 

I believe that setting will affect accuracy by changing the deceleration/acceleration start/stop points... it isn't really an amount of .025" where corner rounding actually takes place.

 

The accuracy of Mastercam is affected by your geometry and total tolerance/filters.